(This G-code is optional and requires a probe)
This G-code is used to set a tool diameter offset.F - Feedrate
Automatic Tool Diameter Offset Measurement function (G35) is used to set the tool diameter (or radius) using two touches of the probe; one on each side of the tool. The first point is set with a G31 block using an M75, and the second point is set with the G35 block. The distance between these two points is set into the selected (non-zero) Dnnn offset.
Setting 63 Tool Probe Width is used to reduce the measurement of the tool by the width of the tool probe. See the settings section of this manual for more information about Setting 63.
This G-code moves the axes to the programmed position. The specified move is started and continues until the position is reached or the probe sends a signal (skip signal).
This code is non-modal and only applies to the block of code in which G35 is specified.
Do not use Cutter Compensation (G41, G42) with a G35.
To avoid damaging the probe, use a feed rate below F100. (inch) or F2500. (metric).
Turn on the tool-setting probe before using G35.
If your mill has the standard Renishaw probing system, use the following commands to turn on the tool-setting probe.
Use the following commands to turn off the tool-setting probe.
Turn on the spindle in reverse (M04), for a right handed cutter.
Also see M75, M78, and M79.
Also see G31.
This sample program measures the diameter of a tool and records the measured value to the tool offset page. To use this program, the G59 Work Offset location must be set to the tool-setting probe location.